Complex manufacturing projects such as the design and manufacture of aircraft generally require the successful integration of design engineering, manufacturing engineering and sometimes numerical control (NC) programing. The production of aircraft, for example, typically requires the successful integration of hundreds of thousands of parts and associated processes according to a comprehensive plan to produce an aircraft in accordance with engineering design data, and includes the automated manufacturing of a number of components, assemblies and sub-assemblies according to NC programming techniques.
Design engineering often makes use of graphic, calculation intensive computer-aided design (CAD) systems to prepare drawings, specifications, parts lists and other design-related elements. In modern CAD systems, component parts are designed by geometrically modeling them in three-dimensions (3D) to obtain a component definition. Designing and developing complex 3D geometry models for many modern aircraft component parts is a powerful but expensive and intricate process where component part performance and design constraints are balanced against manufacturing capability and cost. Manufactures expend large amounts of effort and resources balancing these issues. A key product of this effort is the 3D geometry models of component parts and assemblies of component parts including their respective predefined dimensional tolerances. The bulk of the manufacturing process revolves around efficiently achieving the constraints defined in and between 3D geometry models of component parts and assemblies.
Currently, modern manufacturers expend a significant percentage of their resources to develop and refine 3D geometry models for each component part and assembly. Engineers must then create two-dimensional (2D) drawings to detail, and include dimension and tolerance ranges for the component part features and assembly configurations. This process defines the 2D drawing as the configuration control and the “authority for manufacturing.” This process requires generating a series of 2D perspectives of the components have to be created and, thereafter, the tolerances have to be assigned and detailed on a 2D drawing, where tolerance ranges are assigned based on fit and function of the component part features. For example, in the case of mounting holes centered in two co-planar 1-inch wide flanges that fit alongside of each other, the nominal width dimension is 1.000 inch and the tolerance for the width of the flange should be +0.000/−0.030 inch since positioning two flanges having a width greater than 1.000 alongside each other would cause the centered mounting holes to be shifted further apart from each other and potentially interfere with hole alignment in a mating component. By assigning a tolerance of 1.000+0.000/−0.030 inch the flange width could be machined to a dimension less than 1.000 inch, which would merely leave a gap between the flanges when positioned alongside each other and assembled via the mounting holes.
Thus, for a part flange having a nominal flange width of 1 inch, a 2D part drawing with this assigned tolerance of 1.000+0.000/−0.030 inch would result in the manufacturer setting up machining of the flange at a midpoint of the tolerance, at the dimensional width of 0.985 inches (+0.015/−0.015 inch), to allow for possible manufacturing variations resulting in a width above and below the 0.985 inch width that would nevertheless remain within the 2D drawing tolerance of 1.000+0.000/−0.030 inch.
This process of manufacturing part features to fall within tolerance ranges also typically results in gaps for shimming component parts at assembly, and an inexact definition of the shape of part details; and the resulting component parts or their assembly is then often forced into shape using multiple large tools during manufacturing.
During NC programming and manufacture, NC programs are often designed to machine widths and features of component parts not to nominal dimensions (e.g., 1.000 inch), but rather to a specific dimension within the tolerance range specified in the 2D part drawing (e.g., 1.000+0.000/−0.030), such that manufacturing variations would nevertheless remain within the 2D drawing tolerance to mitigate risk of nonconformance.
NC machining tools could also be set up to machine holes or features to one end or another of their various dimensional tolerances to allow for wear and maximize the usefulness of tools used to machine the parts, or reduce machining time. For example, instead of a nominal size for a hole to be machined, a machinist may install a hole-forming tool or drill bit of a size that is within the tolerance but shifted towards one end of the tolerance range, which would result in hole diameters that initially are at one end of the tolerance range, and as the drill bit wears the resulting hole diameters shift towards the other end of the tolerance range, such that a maximum number of parts may be produced using the drill bit as it gradually wears and the hole diameter changes but remains within tolerance, to thereby prolong the time before the drill bit needs to be replaced with another drill bit.
In another example, the path of a milling machine may be programmed to mill to a minimum pocket depth allowed to remain in tolerance, which may reduce the number of repeated machine tool path passes needed to achieve a pocket depth that is within the tolerance range during the machining process. This in turn may reduce the total machining time and could reduce the risk of thin-wall cracking to mitigate the risk of nonconformance.
After manufacturing component parts, conventional manufacturing techniques are used for assembling component parts to produce assemblies, some of which may be sub-assemblies for even larger assemblies. Traditionally this process has relied on fixtured tooling techniques that force component parts into certain positions and temporarily fastens them together to locate the parts relative to pre-defined engineering requirements. For component parts joined and secured together by fasteners, the assembly process also typically involves pre-drilled pilot holes in one of the joined parts, and a final-hole-size drill jig to drill out the pilot holes and through the other of the joined parts, to thereby produce holes of the desired final size in both parts.
The use of the aforementioned shimming, as well as the locating fixtures and final-hole-size drill jigs during assembly is costly, and often results in a high-level of nonconformance that must be repaired. The traditional assembly process also often involves use of multiple shims, which also adds cost and time. Some techniques have been developed that involve scanning component parts after assembly, and then programming each mating part (customized to a single assembly) to exactly match the surface. But this requires the repeated assembly and disassembly of the component parts to complete the assembly process.